Milling aluminum

Discussion about the CNC Shark Pro Plus HD

Moderators: sbk, al wolford

Re: Milling aluminum

Postby Glug » Wed Mar 05, 2014 2:26 pm

sk8nmike wrote:
Glug wrote:And what is your saw blade good for after a foot or so of that 3/4" plate? Hammer and chisel will work too, but a band saw with a metal cutting blade or a plasma cutter are much better choices.


I'm not sure why people insist on giving opinions on topics they clearly know nothing about.

Very few bandsaws, even large bandsaws, are large enough to cut up large plates of aluminum. The throat clearance tends to be small, and the tables are smaller. 4'x4' sheet? Forget it! A plasma cutter leaves a large heat affected zone, and a rough cut. Yawn.

On the table saw, my cuts were parallel within .010", and extremely clean.

Anyway, I completed my recent aluminum project. It went very well. The shark cuts aluminum much better than it does rock maple. The aluminum has the advantage of carrying away the heat of the cut in the chip. The cutter doesn't even get warm.
Glug
 
Posts: 31
Joined: Fri Feb 15, 2013 10:10 am

Re: Milling aluminum

Postby milo30 » Wed Mar 05, 2014 2:31 pm

Which bit did you use and what kind of feed and speeds did you find that worked the best?
milo30
 
Posts: 553
Joined: Mon Mar 12, 2012 9:21 pm

Re: Milling aluminum

Postby pjmayer » Fri Mar 07, 2014 9:42 am

Glug wrote:The results were mixed - encouraging, but not good. And sometimes frightening. Light cuts, in the .015-.025" range, tend to be the rule to the non-rigid nature of the machine. Sticking with smaller end mills, 3/16 to 1/4, is strongly advised. Solid carbide is a must for stiffness, and also for the typical min router RPMs (my min is 10K).


I tried cutting aluminum one time, and I mostly agree with everything said before. The picture shows how it turned out. The bit was a single O-flute, 1/4" OD, without any spiral. The rough cut was done at 20 in/min. I cut .015" per pass and set the z-axis speed to 5 in/min. The final pass removed .010" to clean things up. This pass was also travelling 20 in/min, but stepped down z=.050" per pass. It took forever. The surface finish in the picture improves towards the bottom because I started out too fast.

This took 2 bits. The first one was carbide and snapped (before I reduced the z-axis speed). The second bit was high-speed steel and a little dull. It changed color from the heat. I will try some sort of coolant next time, but I don't want to wreck my MDF work surface. I was thinking a cold stream of compressed air might help a little.

I think going to a bit with more flutes will hurt more than it helps. The chip load recommendations I've seen for aluminum routing are usually between .002 and .006 inch/rev depending on the bit. In my case, I was (20 in/min)/(10,000 RPM X 1 flute) which equals .002 for a chip load. Adding more flutes would shift this way outside the recommended range. Would this make the bit run hotter?
Attachments
DSC_0548s.jpg
center hole cut on Shark Pro Plus HD
pjmayer
 
Posts: 11
Joined: Mon Aug 23, 2010 11:09 am

Re: Milling aluminum

Postby rungemach » Fri Mar 07, 2014 11:02 am

A good discussion of aluminum cutting so far.

Here is what I have found works for me.

I use an up-spiral 2 flute .250 dia carbide bit. Straight flute bits tend to chatter with these hard materials. (and don't clear chips well either)
Depth of cut per pass is .02 - .03 inches ( yes, thats a LOT of passes) travel speed is 20 ipm and plunge speed is 20 ipm.
rpm is 8000-12,000. definitely not full router speed. The cut is done dry with no lubricant. all of the cutting is done at the tip of the bit, but tool life is still acceptable but not optimal.

YOU MUST RAMP THE CUTS.

A straight plunge at any speed is asking for problems. These bits were meant to cut while traveling, not plunging.
I try and use a 1 inch long ramp. Setting the plunge ipm the same as the feed ipm lets the machine transition from ramp to straight cut without a speed change (smoother)

cutting aluminum is possible , but painfully slow to get good cuts. I would not suggest a Shark for someone that wants to cut these hard materials often, but for a project or two now and then, it can work if you take the time to get the cutting parameters dialed in. If you want to get the best surface quality , I suggest cutting the main passes .005 larger than desired and follow up with a single full depth pass at the true size. you can do this with the same toolpath if you make the tool diameter larger for the "roughing" passes and true size for the finish pass.

attached are some pictures of a aluminum router clamp during cutting and afterwards. these were done with no finishing pass.

cutting clamp.jpg
aluminum during the cut


router clamp.jpg
aluminum router clamp vs plastic
rungemach
 
Posts: 459
Joined: Mon Aug 02, 2010 8:24 am
Location: Sarasota, Florida

Re: Milling aluminum

Postby Glug » Wed Mar 26, 2014 9:48 am

rungemach wrote:Here is what I have found works for me.

I use an up-spiral 2 flute .250 dia carbide bit. Straight flute bits tend to chatter with these hard materials. (and don't clear chips well either)
Depth of cut per pass is .02 - .03 inches ( yes, thats a LOT of passes) travel speed is 20 ipm and plunge speed is 20 ipm.
rpm is 8000-12,000. definitely not full router speed. The cut is done dry with no lubricant. all of the cutting is done at the tip of the bit, but tool life is still acceptable but not optimal.

YOU MUST RAMP THE CUTS.


Mostly the same here. 3/16 or 1/4" 2 flute. I never use a cutter in different materials, even if it is the same model tool - aluminum bits are dedicated to alum, wood for wood, plastic for plastic. The Atrax bits from Enco work well and are inexpensive, especially when they are having a 20% off sale on top of a bit sale.

I am uncertain whether a spritz of lube helps between passes. Whether in improved tool life, or surface finish. I tend to believe it improves the finish. An air jet may also help to cool the tool and prevent chip re-machining.

Regarding ramps, it depends on the type of cut. My most recent project required facing some mounting plates. In that case I chose to use a raster toolpath that resulted in all Z moves happening while outside the piece. So ramps were not necessary. I felt that approach was better than ramping on the piece. In situations where that is not possible, I agree that ramps are essential.

As you stated, with ramps your plunge rate must match the feed rate. If they are different, you risk abrupt changes in feed rate that can shake the machine.

The shark is very wobbly along the Y axis. When you move the Y, you can see it jiggle. You can feel it with your hand, or you can measure it with a dial indicator. So I try and avoid cuts that move the Y and instead leverage the greater stability of the X. So this often dictates raster toolpaths with the primary motion along the X. Also, in this project I extended the tool path far enough outside the workpiece that the Y gantry shake from step-over had stabilized before the material was engaged on subsequent passes.

The results in this particular project were excellent. This was just facing. The holes were made on a drill press. Covering the table with rags makes cleanup easy. Though I prefer the larger chips of aluminum over the fine dust of wood, but wood does smell better.
Attachments
P1300197.JPG
P1300211.JPG
Glug
 
Posts: 31
Joined: Fri Feb 15, 2013 10:10 am

Re: Milling aluminum

Postby DougE » Sun Mar 30, 2014 7:34 am

To rungemach;

Do you happen to have the file for the router mount you machined ?

I am intending to mill my own aluminum after the next project for a Shark Pro HD.

I'd appreciate if you could post it.

Thank you

Doug E
DougE
 
Posts: 43
Joined: Sat Oct 06, 2012 12:37 pm

Re: Milling aluminum

Postby rungemach » Wed Apr 02, 2014 5:03 pm

Doug

Here is a dxf drawing file. you can use the profile for the inner hole which has the recesses to fit the porter cable routers.

This is the same profile that was sent to Sam at Dixie billet,
who makes these clamps out of thicker billet aluminum, and sells them for around fifty bucks.

Differences from the stock clamp, besides material, is that the recesses for the router side pins are a bit deeper than the factory recesses to prevent the router from riding on the pin and not getting a good "full body grip" on the router body. The factory one I had for a sample was held from tightening on the body by the router pins, so I made the recesses deeper.
Also, the tab for the pinch bolt is also beefier.

When I make something like this , I will just spot the locations for the drilled holes by using an 1/8" drill bit and touching the surface , maybe .040 deep. Then go to a drill press to drill the hole. The shark does not like drilling aluminum.
Attachments
HD router mount drawingr3.dxf
(52.8 KiB) Downloaded 162 times
rungemach
 
Posts: 459
Joined: Mon Aug 02, 2010 8:24 am
Location: Sarasota, Florida

Re: Milling aluminum

Postby DougE » Thu Apr 03, 2014 3:09 pm

Thank you very much 'rungemach' for sharing the dxf. file.

This will come in handy soon as I expect to be breaking down the Shark and finally putting it into an enclosure.

Again, I, and it looks like collective 'we' appreciate your sharing.

Thank you kindly

Doug E
DougE
 
Posts: 43
Joined: Sat Oct 06, 2012 12:37 pm

Re: Milling aluminum

Postby rungemach » Thu Apr 03, 2014 3:28 pm

Info on Sams clamp can be found here.

viewtopic.php?f=2&t=3314&p=19037

a bit over 50 bucks inc shipping.
( disclaimer, I make no money from his clamps, he is a separate business)
Sam has made other aluminum parts for me, but not shark clamps. Very nice guy to work with.

I believe he is making them in aluminum over 1" thick, which would be hard to do on a shark.
I have found 1/2 inch aluminum will work pretty well, but thicker is better...
on my routers I use two 1/2 inch thick clamps with a separation between. but that is a modified z axis design.
rungemach
 
Posts: 459
Joined: Mon Aug 02, 2010 8:24 am
Location: Sarasota, Florida

Re: Milling aluminum

Postby rossjonnes » Thu Feb 06, 2020 5:21 am

Who has been able to sample the various products on this list and can be able to pick out the best one? https://onlychainsaw.com/best-chainsaw-chain/
rossjonnes
 
Posts: 1
Joined: Fri May 31, 2019 1:29 am

Previous

Return to CNC Shark Pro Plus HD

Who is online

Users browsing this forum: No registered users and 2 guests